problem about ADE simulation

EDAboard.com Forum Index -> Analog IC Design & Layout -> problem about ADE simulation

Author

Message

oversea

Joined: 15 Oct 2009
Posts: 2

15 Oct 2009 7:32 problem about ADE simulation

Hello

I was using cadence IC5141 with IBM PDK. Somehow I couldn't run simulation anymore because the instances are not defined. For example, if I instantiate a mim capacitor, the edit property form tells me subcircuit name is "mim", but in netlist, the model name becomes "subcircuit", I guess this is the reason prevents me from simulation further. Anybody could help me out? Thanks a lot.

dick_freebird

Joined: 04 Mar 2008
Posts: 313
Helped: 46
Location: USA

15 Oct 2009 15:01 problem about ADE simulation

There should be an instance of the MIM element and it may
be a subcircuit call that requires a subcircuit definition,
but both should be there. Perhaps you skipped over the
instance line, or perhaps there is some netlister issue
(like missing property?) that inhibits the netlister from
outputting the instance line. Look at the various output
windows for error complaints (CIW?).

It's common for there to be multiple subflows and maybe
there is a master variable that calls out whether you are
going to have MIMs in the flow or not; maybe that inhibits
MIM from netlisting. Just conjecture, there.

Try making a bone simple test circuit (like MIM,
resistor
and voltage source) and post up the intermediate and final
netlists. Sometimes there are schemes where the subcircuit
and instance are done by one call, though I have not
seen this used since cdsSpice went bye-bye.

oversea

Joined: 15 Oct 2009
Posts: 2

15 Oct 2009 21:42 problem about ADE simulation

Below is my netlist, I just used one resistor with one capacitor.
Obviously the model name for resistor and capacitor are both "subcircuit". If I change capacitor to "mim" manually, e.g., I can run through simulation.

// Generated for: spectre
// Generated on: Oct 15 14:23:13 2009
// Design library name: test
// Design cell name: test2
// Design view name: schematic
simulator lang=spectre
global 0
include "/opt/cadence/ic5141/tools/dfII/samples/artist/ahdlLib/quantity.spectre"

// Library name: test
// Cell name: test2
// View name: schematic
V0 (net13 0) vsource dc=1
OPppc0 (net18 0 net20) subcircuit r=3.76926K w=200.00n l=1.6u m=1 sbar=1 \
pbar=1 bp=0 rsx=50
CM0 (net18 net13 net20) subcircuit l=8u w=11.08u c=91.8836f m=1 bp=2 est=1 \
setind=-2 rsx=50 dtemp=0
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
checklimitdest=psf
dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
dcOpInfo info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts where=rawfile
saveOptions options save=allpub currents=all

Added after 4 minutes:

Problem solved. I missed one line: export CDS_Netlisting_Mode=Analog in my bashrc file. Though I don't know what it means but it does help.
Thanks a lot.